06/06/2017

How to Cross-Reference Dimensions between Parts in an Assembly

CATIA offers an unparalleled ability for designing parts in the context of other parts in an assembly. While linking geometrical elements between the parts designed in context is a well-known technique (and is taught in the Rand 3D training class “CATIA Advanced Assembly Design and Management”), the option to cross-reference dimensions between the parts if often overlooked.

In this post, I will explain how to drive dimensions in one part using dimensions from another part in an assembly. As an example, we will work with the assembly consisting of the T-bar for the trailer hitch and the pull pin. The task is to ensure that the diameter of the hole in the T-bar is always 0.5mm greater than the diameter of the pin.

First, we need to ensure that the link between the dimensions will be maintained throughout the design process. In the top-level menu, select Tools > Options, then go to the Infrastructure > Part Infrastructure section, and in the General tab, select the Keep link with the selected object option. Click OK to close the Options dialog box when done.

Next, we will locate the dimension that controls the diameter of the pull pin. This will be the driving dimension in our design.

Hide the T-bar part and double-click the pin part in the tree to activate and to switch to the Part Design workbench.

Note that the base feature for the pin is Rib.1. Double-click Rib.1 in the tree to open the Rib Definition dialog box, and note that Sketch.2 was the profile extruded along the center curve Sketch.1 to create the pin. Apparently, Sketch.2 should contain the dimension that controls the diameter of the pin. Select the Sketch icon near the Sketch.2 field to enter the Sketcher workbench.

Note that there is only one dimension in the sketch, which is the 15mm diameter of the circle.

Now we have to find out the internal name of the parameter that controls this dimension. In the Knowledge toolbar, click the Formula icon. Once the Formulas dialog box opens, click Sketch.2 in the tree 1st (this ensures that only parameters belonging to Sketch.2 are shown in the list), then click the D15 dimension in the sketch. The Formulas dialog box displays as shown below.

Note that this dimension has a rather long internal name, which is PartBody\Sketch.2\Radius.9\Radius. In general, the internal parameter names in CATIA are built as backslash-separated paths from parent to child, which actually helps in identifying which feature a particular parameter belongs to.

Another observation you might find interesting is that this diameter dimension is actually stored as a radius parameter in CATIA. In fact, all diameter dimensions in CATIA sketches are internally stored as radius parameters. We will need to take that into account when linking dimensions of the pin and the hole.

Click Cancel to close the Formulas dialog box, and exit the Sketcher and the Rib Definition without making any changes.

Next, we will go into the T-bar model, and create a relation between the hole diameter and the pin diameter.

Hide the pin part and double-click the T-bar part in the tree to activate and to switch to the Part Design workbench.

Select the hole in the model, and note that Hole.1 highlights in the tree (another way to find the feature in the tree would be to use the Center graph option in the contextual menu). This is the feature used to create the hole.

Double-click Hole.1 to edit. In the Hole Definition dialog box that opens, right-click in the Diameter field, and select Edit formula in the contextual menu.

While in the Formula Editor dialog, go to the pin part, and select Sketch.2 in the tree. The External parameter selection dialog box opens, displaying all the parameters belonging to Sketch.2 in the pin part. Highlight Radius.9\Radius in the list (this is the pin radius parameter, as we had determined earlier) and click OK.

The selected external dimension gets automatically inserted into the formula, and the Formula Editor dialog box now displays as shown below.

Taking into account that the pin dimension is a radius parameter, as well as to accommodate the requirement of 0.5mm clearance between the pin and the hole, modify the formula as show below. Click OK when done, then close the Hole definition dialog box.

We’re done! Now, whenever the pin diameter is changed and the assembly is updated, the hole diameter will also change accordingly.

If you’re curious how this all works, go ahead and examine the links between the parts. With the T-bar part active, select Edit > Links. The Links of document dialog box opens as shown below.

Note that the parameter in the T-bar part, which is the diameter of the hole, is now linked to the sketch dimension in the pin part. You can think of a link in CATIA as of a “transmitter of information”, so when the pin dimension is changed, the information about the change is automatically transmitted into the T-bar part. In other words, using the links, we’ve just relegated to CATIA the responsibility of maintaining the design intent, instead of having to do this ourselves.

In my next post, I will explain how to use Publications to cross-reference dimensions in CATIA, which yields a huge advantage over the method described above.